PDA

View Full Version : [IMG] Turning threads in steel: badly torn finish with ground and honed HSS



Oyvind Ryeng
11-09-2017, 05:09 PM
http://oyvindryeng.net/img_host/thread.jpg

Pictured is a typical example from today, M16x1.5 near side, M18x2.5 far side. Regular, round turning with carbide inserts leave a very beautiful finish most of the time, and also when threading with 11IR carbide inserts held in boring bars. This is on my nearly 2 metric ton 1980 TOS SN50B x 1500 mm. from the wonderful socialist paradise state of Czechoslovakia (now defunct).

I try to be careful with workpiece overhang and often use the tailstock for support. The problem only exist in general purpose low carbon steels S235, S275, S355 and St. 52, equivalent to about AISI 1018 through ASTM A36 and A572 grade 50; I've not yet had the pleasure trying to thread stainless steel or the chromium-molybdenum kinds. Almost all the work I do is in mild steel, and the thread cutting problem does not manifest in aluminium or brass at all, that I've seen. I'm using flank infeed at 29.5° angle as measured off the X-axis and near ~0.05-0.02 mm. finishing infeed dialed in on the compound slide. I'd like to try some lead/sulfur free-machining steel, but have none at hand that I can readily identify with certainty.

I've got the threading tool ground with around 10° side rake, no back rake and what I believe to be a generous side relief angle, yet still I'm leaning towards the possibility of not having enough relief angle on the tool? I guess more experimentation is on the agenda for the next 5-year plan.



Bonus round: I know you gentlemen love seeing pictures of our decadent filth and depraved equipment hoarding, so here's a recent one, showing my new old 1.4 ton TOS BPH 20 surface grinder from 1975 and the rear of my 1956 Ferguson 35 tractor with the 2.3-liter 4-cylinder Standard Motor Company diesel engine. The surface grinder was supplied with a magnetic chuck from Eclipse in England, an external coolant pump and tank and also three 250 mm./10-inch grinding wheels, one of which I've been able to identify as for grinding hardened steel. It's blueish in color, and two others are vitrified, open structure and pink.

http://oyvindryeng.net/img_host/workshop.jpg

J Tiers
11-09-2017, 05:17 PM
Soft gummy steel can do that.

MattiJ
11-09-2017, 05:18 PM
A. What cutting oil you are using when threading? Spindle rpm?
B. Can you post pic of your HSS threading tool? It needs to be absolutely sharp.

Solution C. is to buy cheapish 16ER carbide inserts and tool holder but this HSS thing should be sorted out also..
https://www.ebay.com/itm/10PCS-IN-BOX-MITSUBISHI-MMT16ER-AG60-VP15TF-Carbide-Insert-New/222359170714?epid=581302883&hash=item33c5a3ae9a:g:smYAAOSwmmxW6SPU

Oyvind Ryeng
11-09-2017, 05:26 PM
Using CRC Supercut II cutting fluid.
Speed was about 125 RPM.
Good call on this perhaps being a material problem.
Great call on getting more tools, I've been looking at a 16ER solution for some time now.
Cutting tool is honed with a diamond lap to a appreciably bright cutting edge.

CRC Supercut II (http://uk.rs-online.com/web/p/lubricants/7805338/)

EDIT: Tool pictures tomorrow, will dust off my macro lens for my DSLR.

J Tiers
11-09-2017, 05:40 PM
...
Cutting tool is honed with a diamond lap to a appreciably bright cutting edge.
,,,,

I suspect I know what you mean, but just in case; a sharp edge actually disappears. It is only dull edges that show any shiny or bright line etc at the actual edge itself.

MattiJ
11-09-2017, 05:40 PM
Supercut II is what I was also using until I get allergic to it. Speed sounds reasonable but you could try and see what happens if you drop the speed really slow.

Material is part of the problem but in my experience the VP15TF coated Mitsubishi inserts work very nicely also on S355 cold drawn bar stock that is common here in Europe.

If you hone hand-held with diamond lap its also possible that you get slight radius on the cutting edge so that its not really sharp. Depends how good your technique is. I have seen it happen to "my friend" but I'm of course not such a clumsy bastard. :rolleyes:
Or your HSS is some crap quality chinese import, "my friend" had also that.

Toolguy
11-09-2017, 06:16 PM
You might try to find the local equivalent of 1215 alloy. It's the easiest, cleanest cutting low carbon steel I've found so far.

lakeside53
11-09-2017, 08:31 PM
or any of the leaded steels, like 12L14 etc

10KPete
11-09-2017, 09:03 PM
My take is that the tool needs about 10* of top rake for this gummy stuff. That's been my experience anyway. I have a tool for this stuff with the top rake going away from the left cutting edge. I don't care much about the right 'cutting' edge because it never cuts! With the compound at 29.5* I feed in with the compound only thus I'm always cutting with a high rake tool. The old lard/sulfur oil is my go to for this. Good threads every time...

Cheers,
Pete

MrWhoopee
11-09-2017, 09:13 PM
Definitely related to the material, it looks just like threading cold rolled steel at low speeds. Several things occur to me:
1. Increase RPM (I know, it gets scary).
2. Sulphurized cutting oil.
3. Stress relieving or annealing with a torch.
4. Using hot-rolled 1020, 1215, 12L14 (if it's still available), 1144 (Stressproof), or even 303 stainless.
5. Lapping the tool seems like over-kill and may be counter-productive. The fine grooves in a ground cutting edge can act as tiny chip breakers.

754
11-09-2017, 09:52 PM
I was thinking top rake too .. it looks like its not cutting freely..
What method do you use for centre height ?
I feed straight in on all my threading and finish is rarely an issue.

danlb
11-09-2017, 10:01 PM
It seems to me that you might be cutting too shallow. Look at the page https://www.sandvik.coromant.com/en-gb/knowledge/threading/thread_turning/formulas_and_definitions/pages/default.aspx to see what Sandvik recommends.

In the case of the 1.5 mm pitch, Sandvik was calling for 6 passes of decreasing depth, starting with .23mm and finishing with .010mm.

Dan

MattiJ
11-10-2017, 03:23 AM
or any of the leaded steels, like 12L14 etc

12L14 or 1215 equivalents are hard in here to find. Hardly anyone stocks it or is willing to deal with small customers.

Calcinated Imatra M-steels are reasonably nice to work with:
http://www.ovako.com/Products/M-Steel/
Imatra 4M ( close to 1045), or MOC 410M (4140 prehard)

boslab
11-10-2017, 07:01 AM
Nothing wrong with it lovely bit of rebar.
Looking at the marks it looks almost like a chatter type of thing as well, tool rigid?
Mark

Mcgyver
11-10-2017, 08:29 AM
well it is why they call 12L14 screw stock - I can be difficult getting good finishes with the broad cut threading requires, in gummy materials. The only way I've been able to get through tear out like that in threading is super sharp hss tools - not quite a mirror as a wood worker would but almost - head in the that direction. Use heavy cutting oil, light cut and as slow as the lathe will go. Slow is the key, with oil and a super sharp tool.....think of scraping, where a super sharp tool going very slowly will make a shiny cut in otherwise difficult to machine steels. My suggestion is toward trying to replicate those cut dynamics

vpt
11-10-2017, 08:46 AM
I'd agree with the top rake and super sharp hss. No top rake many times material seems to just be "smeared" off the parent part leaving a rough finish. I also find sometimes if you have enough clearance setting the toop slightly above center will produce a better finish.


The absolute best finish I have ever seen strait off the tool was in titanium. Like a mirror!

https://i.imgur.com/oMcH6Tk.jpg

MattiJ
11-10-2017, 08:47 AM
well it is why they call 12L14 screw stock - I can be difficult getting good finishes with the broad cut threading requires, in gummy materials. The only way I've been able to get through tear out like that in threading is super sharp hss tools - not quite a mirror as a wood worker would but almost - head in the that direction. Use heavy cutting oil, light cut and as slow as the lathe will go. Slow is the key, with oil and a super sharp tool.....think of scraping, where a super sharp tool going very slowly will make a shiny cut in otherwise difficult to machine steels. My suggestion is toward trying to replicate those cut dynamics

Hear hear.
Dealing with BUE (build up edge) and tearing it helps to go either really slow or really fast. The "really fast" for soft gummy materials is probably not realistic for manual lathe threading as it might be something like 200...400m/min.

mars-red
11-10-2017, 08:58 AM
I've been there myself, the material isn't easy to get a nice finish, but it shouldn't be difficult to do better than what you're showing. Assuming the geometry of the tool is sorted out, and that it has a truly sharp edge, then start to look at your depth of cut for the final passes. You'll want them to be really shallow, and follow the final one with several spring passes. My final pass before making some spring passes is usually 0.02mm or less. Also, for threads this size in this sort of steel, you'll want to make sure you're feeding in via the compound slide set at about 29 degrees, rather than plunging straight in. The chatter in your photos really looks like the threading tool was feed straight into the work, but it could have had other causes (such as depth of cut or tool geometry).

J Tiers
11-10-2017, 09:12 AM
Rake on the tool will change the geometry, and can require different angles.

The simple case is if you use rake across the tool, so the left edge is not changed, and the right edge is not asked to cut at all, in which case you do not need to consider the angles aside from the normal angle of left edge.

mickeyf
11-10-2017, 01:17 PM
I feed straight in on all my threading

Not my experience.

As J Tiers says, "right edge is not asked to cut at all" --feed in at an angle with your compound so that only the left edge of the tool is cutting and needs to be considered as having correct geometry. If both left and right were cutting their chips would collide, and you can't possibly have the same rake on both without pretty fancy grinding equipment.

HWooldridge
11-10-2017, 02:38 PM
Rigidity also helps. I used to get the same type of results on my old Sheldon 10x36 with the stock lantern post setup. I sold the Sheldon and bought a much newer Jet 12x36 with an Aloris QCTP setup and the problem went away. This was using the same cutting tools and steel source.

J Tiers
11-10-2017, 03:09 PM
Rigidity also helps. I used to get the same type of results on my old Sheldon 10x36 with the stock lantern post setup. I sold the Sheldon and bought a much newer Jet 12x36 with an Aloris QCTP setup and the problem went away. This was using the same cutting tools and steel source.

As the OP is using a "Multifix" toolpost, that is unlikely to be a problem. Look closely at the pic of his shop.

Oyvind Ryeng
11-10-2017, 04:36 PM
I suspect I know what you mean, but just in case; a sharp edge actually disappears. It is only dull edges that show any shiny or bright line etc at the actual edge itself.
Right you are, I of course ment that the area just below/adjacent to the cutting edge was honed/brightened up. The cutting edge itself is in my eye sharp enough to not reflect light.


Supercut II is what I was also using until I get allergic to it. Speed sounds reasonable but you could try and see what happens if you drop the speed really slow.

Material is part of the problem but in my experience the VP15TF coated Mitsubishi inserts work very nicely also on S355 cold drawn bar stock that is common here in Europe.

If you hone hand-held with diamond lap its also possible that you get slight radius on the cutting edge so that its not really sharp. Depends how good your technique is. I have seen it happen to "my friend" but I'm of course not such a clumsy bastard. :rolleyes:
Or your HSS is some crap quality chinese import, "my friend" had also that.
I'm sorry to hear about your allergy to the cutting fluid. I haven't tried them all by a long shot, but the CRC stuff seem to work well for me. I've tried cutting speeds on workpieces 16-20 mm. OD (5/8" ~ 3/4") from 45-355 RPM, seemingly without much difference in the cutting action. Good call on the Mitsubishi inserts, I have a lot of inserts from them already and the quality is quite good. I'm very careful when lapping and at all cost avoid dulling the cutting edge in somewhat of a chamfering maneuver. I do have a lot of HSS tool steel from the far east, specifically that one unmentionable country, but most of it holds an edge well for general turning and profiling. I'm careful with the cutting speed, though.


You might try to find the local equivalent of 1215 alloy. It's the easiest, cleanest cutting low carbon steel I've found so far.
I'd love to try some one day.


My take is that the tool needs about 10* of top rake for this gummy stuff. That's been my experience anyway. I have a tool for this stuff with the top rake going away from the left cutting edge. I don't care much about the right 'cutting' edge because it never cuts! With the compound at 29.5* I feed in with the compound only thus I'm always cutting with a high rake tool. The old lard/sulfur oil is my go to for this. Good threads every time...

Cheers,
Pete
Thanks for the tip. I already use a tool with side rake, but have not tried using any back rake, or a combination thereof. It very well could be something for me to look into. I eyeballed the rake angle I'm currently using, and it actually appears a lot closer to 15° than 10.


Definitely related to the material, it looks just like threading cold rolled steel at low speeds. Several things occur to me:
1. Increase RPM (I know, it gets scary).
2. Sulphurized cutting oil.
3. Stress relieving or annealing with a torch.
4. Using hot-rolled 1020, 1215, 12L14 (if it's still available), 1144 (Stressproof), or even 303 stainless.
5. Lapping the tool seems like over-kill and may be counter-productive. The fine grooves in a ground cutting edge can act as tiny chip breakers.
Thanks for the tips. I've tried having the tool upside-down and threading away from the headstock when making right-hand threads, but maybe I haven't used a high enough speed? Sulphurized cutting oil is on my shopping list already, but haven't tried it yet. (Reverse) heat treatment; would not that make the material even more gummy? I believe I'll continue to lap my cutting edges, if not for anything else, it reduces the tendency to form a built-up-edge.


I was thinking top rake too .. it looks like its not cutting freely..
What method do you use for centre height ?
I feed straight in on all my threading and finish is rarely an issue.
No top rake yet, only side rake. Maybe I'll try adding some top rake at a later time. The center height gets set by pinching my 150 mm. long, thin ruler between the cutting edge and the workpiece. I believe flank infeed at an angle is the way to go, and especially for more coarse threads.


It seems to me that you might be cutting too shallow. Look at the page https://www.sandvik.coromant.com/en-gb/knowledge/threading/thread_turning/formulas_and_definitions/pages/default.aspx to see what Sandvik recommends.

In the case of the 1.5 mm pitch, Sandvik was calling for 6 passes of decreasing depth, starting with .23mm and finishing with .010mm.

Dan
Yes, I've tried fine infeeds for finishing, and will often dial in 0.20 - 0.25 mm. for the "roughing" passes to start with, and reduce the infeed as I progress. I'm actually already making 1.5 mm. pitch threads in 5-8 passes, depending on how I hit/miss the mark for sizing near the end of the threading cycle.


12L14 or 1215 equivalents are hard in here to find. Hardly anyone stocks it or is willing to deal with small customers.

Calcinated Imatra M-steels are reasonably nice to work with:
http://www.ovako.com/Products/M-Steel/
Imatra 4M ( close to 1045), or MOC 410M (4140 prehard)
Ovako is quite high quality I've heard, but never seen it for sale here in Norway. I guess I can order some and have it delivered to the border town of Kilpisjärvi perhaps.


Nothing wrong with it lovely bit of rebar.
Looking at the marks it looks almost like a chatter type of thing as well, tool rigid?
Mark
Rebar, huh? The workpiece I've been having a hard time with recently is a 20 mm. OD hard-chromed shock absorber rod, most likely even from a Volvo passenger car. I'll have you know, my good Sir, that both me and my lathe is very much above turning just any kind of junk and road-side trash, I only use the highest quality of free, surplus, gifted, begged-for, inherited, found, stolen, and/or recycled "Mysterium Stahl" ™.


well it is why they call 12L14 screw stock - I can be difficult getting good finishes with the broad cut threading requires, in gummy materials. The only way I've been able to get through tear out like that in threading is super sharp hss tools - not quite a mirror as a wood worker would but almost - head in the that direction. Use heavy cutting oil, light cut and as slow as the lathe will go. Slow is the key, with oil and a super sharp tool.....think of scraping, where a super sharp tool going very slowly will make a shiny cut in otherwise difficult to machine steels. My suggestion is toward trying to replicate those cut dynamics
I believe I've tried this approach already without much success, but perhaps I'm not sharpening the tool enough? Not fine enough infeed? I'll do try to get some other cutting oil, but the CRC I'm already using works well for other turning operations using the same HSS toolbits.

[END OF PART 1, PART 2 WILL FOLLOW WITH MORE COMMENTS AND PICTURES]

Oyvind Ryeng
11-10-2017, 04:41 PM
I'd agree with the top rake and super sharp hss. No top rake many times material seems to just be "smeared" off the parent part leaving a rough finish. I also find sometimes if you have enough clearance setting the toop slightly above center will produce a better finish.


The absolute best finish I have ever seen strait off the tool was in titanium. Like a mirror!

Nice threads right there. I have not tried cutting above center because I'm afraid to run out of clearance and start smearing and rubbing. I do have tried to set the tool below center without any appreciable difference to the cut.


Hear hear.
Dealing with BUE (build up edge) and tearing it helps to go either really slow or really fast. The "really fast" for soft gummy materials is probably not realistic for manual lathe threading as it might be something like 200...400m/min.
That's quite fast, yes. Probably not a good idea to even try when near any form of shoulder or tailstock support.


I've been there myself, the material isn't easy to get a nice finish, but it shouldn't be difficult to do better than what you're showing. Assuming the geometry of the tool is sorted out, and that it has a truly sharp edge, then start to look at your depth of cut for the final passes. You'll want them to be really shallow, and follow the final one with several spring passes. My final pass before making some spring passes is usually 0.02mm or less. Also, for threads this size in this sort of steel, you'll want to make sure you're feeding in via the compound slide set at about 29 degrees, rather than plunging straight in. The chatter in your photos really looks like the threading tool was feed straight into the work, but it could have had other causes (such as depth of cut or tool geometry).
I do not believe this is chatter. It makes no such distinctive noise. I have not tried spring passes because I've heard that that is just a crutch / Band-Aid indicative of another problem with the cut.


Rake on the tool will change the geometry, and can require different angles.

The simple case is if you use rake across the tool, so the left edge is not changed, and the right edge is not asked to cut at all, in which case you do not need to consider the angles aside from the normal angle of left edge.
I don't hone the right cutting edge as I'm feeding in at an angle and the right side of the tool does not touch the work at all. I do use a 60° included angle reference guide when grinding the tool to make my flanks straight and in alignment.


Not my experience.

As J Tiers says, "right edge is not asked to cut at all" --feed in at an angle with your compound so that only the left edge of the tool is cutting and needs to be considered as having correct geometry. If both left and right were cutting their chips would collide, and you can't possibly have the same rake on both without pretty fancy grinding equipment.
I agree and will continue to use flank infeed at an angle. I have tried plunging straight in in fine-pitch threads in brass and aluminium without ill effects though.


Rigidity also helps. I used to get the same type of results on my old Sheldon 10x36 with the stock lantern post setup. I sold the Sheldon and bought a much newer Jet 12x36 with an Aloris QCTP setup and the problem went away. This was using the same cutting tools and steel source.
Oh, I'm quite rigid already. A two ton Czech lathe and a Multifix "B"-size QCTP from Wuhan Create Tool in China. I sometimes do hogging in 3-4" diameter mild steel with parameters along these lines: 700-1000 RPM, feeding 0.30 - 0.40 mm./rev, taking up to 4-5 mm. depth of cut (removing 8-10 mm. of the diameter). The lathe does not make a squak, except for the loaded sound of the motor. It consumes around 17A @ 230V 3-phase at idle, and peak loads near 35A when roughing would by my math have the active power approach ~15 horsepowers at most.


Cutting edge as presented to the workpiece. It's ground at an all-around 9-degree offset to have the cutting edge approach close to the chuck without shearing the drive pin on the threading leadscrew for the fourth time.
http://oyvindryeng.net/img_host/threading/01.jpg

Front view of the toolbit:
EDIT: the toolbit is 10 mm. square, or midways between 3/8" and 7/16":
http://oyvindryeng.net/img_host/threading/02.jpg

The lapped cutting edge, viewed from below:
http://oyvindryeng.net/img_host/threading/03.jpg

More of the imperfect finish, this is with a fresh grind and hone on my toolbit:
http://oyvindryeng.net/img_host/threading/04.jpg

Oyvind Ryeng
11-10-2017, 04:41 PM
Lowered the cutting tool:
http://oyvindryeng.net/img_host/threading/05.jpg

Lowered it some more and reduced the speed to 45 RPM and a very fine infeed:
http://oyvindryeng.net/img_host/threading/06.jpg

100% crop of the picture above from my Olympus E-3 with Zuiko 50 mm. f/2.0 macro lens. The surface is brutal enough to be a death-metal album cover:
EDIT: It looks like a scaly dragon is wrapping itself around a round rod. A small dragon, to be sure, with a diameter of 1.5 mm.
http://oyvindryeng.net/img_host/threading/07.jpg

This is with an 11IR carbide insert boring bar, upside-down and threading away from the chuck at the same slow 125 RPM:
http://oyvindryeng.net/img_host/threading/08.jpg

Oyvind Ryeng
11-10-2017, 04:42 PM
Speeding it up:
http://oyvindryeng.net/img_host/threading/09.jpg

Speeding it up again:
http://oyvindryeng.net/img_host/threading/10.jpg

Speeding it up some more (700 RPM):
http://oyvindryeng.net/img_host/threading/11.jpg

Same setup, but something went wrong. Too high DOC, perhaps:
http://oyvindryeng.net/img_host/threading/12.jpg

Oyvind Ryeng
11-10-2017, 04:42 PM
Now trying Mystery Stainless, 96 mm. OD x 1.5 mm. pitch. Excellent result @ 63 RPM. Feeding in 0.20 mm., down to 0.02 mm. when finishing. I got a continuous stringy chip as expected.

http://oyvindryeng.net/img_host/threading/13.jpg

http://oyvindryeng.net/img_host/threading/14.jpg

http://oyvindryeng.net/img_host/threading/15.jpg

Illinoyance
11-10-2017, 05:17 PM
The steel you are using is prone to galled or torn threads when cut at low surface speed. It may not be feasible to run fast enough to get a decent finish. In the shop where my son worked the shop foreman ordered the cheapest steel he could get to make some short shafts. In order to get sufficient speed to cut smoothly the RPM was so high the Z axis servo couldn't keep up, resulting in drunken threads. Try to get a steel better suited for machining. Others have posted their preferences. All are better suited for threading than what you use. Hot rolled and 0.2% carbon are a lousy combination.

Take a tip from pipe fitters. They die cut threads in really gummy steel all the time. They always use dark cutting oil that contains lots of sulfur. They seem to get decent threads at low speeds most of the time. Try the dark oil.

One of my favorite materials to machine is cold finished 1144 (Stressproof). Because of its sulfur content it is not recommended for welding.

MattiJ
11-10-2017, 05:18 PM
I did some test runs on crappiest S355 cold drawn stock they sell around here.
HSS tool with couple of passes with 0.2mm plunging straight in:

https://i.imgur.com/KcU4zID.jpg?1

Nasty nasty... decrease the cutting depth to 0.04mm per rev and 0.02mm for last 5 passes:

https://i.imgur.com/4VAIMD1.jpg?1

The one on the left is turned with HSS tool and the one on the right is turned with ER16 VP15TF carbide insert.
Took probably 3 times longer with the pretty sharp sharp HSS tooling because it was tearing a lot more compared to insert. Insert tool did tear some but it was nowhere near as bad.
On some parts of the thread the finish looks great on the piece turned with HSS tool but there is still tearing marks visible. .The one turned with insert has more constant finish from thread to thread but doesn't look as nice as the piece turned with HSS in the best parts.

Both run @100rpm and last few finishing passes @ 40rpm.

MattiJ
11-10-2017, 05:27 PM
P.S. The part turned with HSS tool is probably already teared too much in the first pic. The tears look rather big and extend deep in to the stock material.
Should have gone with smaller cut of depth right from the start.

PStechPaul
11-10-2017, 05:38 PM
It sure looks like a case of bad material, since the SS turned out so nicely. Have you tried turning or facing the same material? If you have problems with that, it would definitely point to a material problem.

AIUI, setting the compound angle to 29.5 degrees causes the cutting tool to do most of its cutting on the left side, but it also just barely shaves material on the right. If it is set greater than 30 degrees, it will leave steps on the right side for each threading pass. Having the tool ride on the right side also helps with rigidity, as it prevents the tool from springing to the right.

Here is my first attempt ever at threading, 3/8"-16, in a piece of steel (probably 1018):

http://enginuitysystems.com/pix/tools/Single_Point_Threading_0.375-16_1605.jpg

http://enginuitysystems.com/pix/tools/Single_Point_Threading_0.375-16_1606.jpg

http://enginuitysystems.com/pix/tools/Single_Point_Threading_0.375-16_Detail_1605.jpg

This was done on my Harbor Freight 9x20 lathe using a hand-sharpened HSS tool bit. You can see that I may not have had the compound set quite right, so there are ridges for each pass. I think this is the threading tool I used:

http://enginuitysystems.com/pix/tools/Lathe_1618.jpg

lakeside53
11-10-2017, 06:05 PM
At end of your compound passes (less one) do a light simple plunge cut with the tool set at 30 degrees. That will clean it up any ridges etc.

754
11-10-2017, 08:32 PM
Right below your cutting edge, looks like no clearance..
I mean the side toward the chuck.
Side rake on top of tool should be ok, just makes it harder to check with the guage while grinding.

J Tiers
11-10-2017, 09:31 PM
I share the questions with regard to the very edge area where the honing is done. That must still have some clearance rake.

Also, the side is nice, but the top of the tool is not very good-looking. Maybe the edge is not as sharp as it could be as to the top. And also maybe the cut material is not getting away cleanly, and may be getting re-welded onto the part. It does not look like classic re-welding, but ......


At end of your compound passes (less one) do a light simple plunge cut with the tool set at 30 degrees. That will clean it up any ridges etc.

But his back-side edge is obtuse angle, not a cutting angle. So making it try to cut is maybe not so good.

Also, something looks wrong with the pictures. The material that is smeared, looks like it is "smeared forward" with the rotation, and not "smeared back" in the direction the tool should have pushed it against rotation. Otherwise looks a bit like the way a built-up edge tears away.

And again, is the threading tool ground with slight angle to account for the thread helix? It does not always seem as if that would be so important, but.....

Willy
11-10-2017, 09:37 PM
Right below your cutting edge, looks like no clearance..
I mean the side toward the chuck.
Side rake on top of tool should be ok, just makes it harder to check with the guage while grinding.

This what I'm seeing as well, not sure if this is an artifact of the photo or not but this could be responsible for the torn effect left by the tool bit, especially in soft gummy steel. I have found that when cutting these types of steels that just the slightest variation of the cutting edge geometry can make a surprisingly huge difference in finish quality.

I see that the facing cut on the end of the work piece has a much more satisfactory finish. What can you do to the thread cutting tool bit to achieve similar geometry/results?


http://oyvindryeng.net/img_host/thread.jpg

754
11-10-2017, 11:11 PM
Take a piece of bar stock, put it in the chuck.
Now using your threading tool cut a wide chamfer with the tool.
Tell us what happens... if it can do that nicely it won't cut good threads....

MattiJ
11-11-2017, 12:24 AM
Take a piece of bar stock, put it in the chuck.
Now using your threading tool cut a wide chamfer with the tool.
Tell us what happens... if it can do that nicely it won't cut good threads....

I don't get it?

danlb
11-11-2017, 12:28 AM
Take a piece of bar stock, put it in the chuck.
Now using your threading tool cut a wide chamfer with the tool.
Tell us what happens... if it can do that nicely it won't cut good threads....

I think you meant that if you CAN'T do that....


That's not a bad way to try different speeds and infeeds to determine the optimum settings.

lakeside53
11-11-2017, 12:31 AM
But his back -side edge is obtuse angle, not a cutting angle. So making it try to cut is maybe not so good.

.

I was referring to PStechs post above mine. ;)

MattiJ
11-11-2017, 01:22 AM
I think you meant that if you CAN'T do that....


That's not a bad way to try different speeds and infeeds to determine the optimum settings.

Just remember that you need to account for the helix angle. Some of the coarsest standard threads like 1/4-20 UNC have almost 4 degrees helix angle. If you grind the relief angle to 7 degrees you have effectively only 3 degrees relief angle left on the leading edge.

754
11-11-2017, 01:51 AM
What I am saying, is test that edge, see if it works.

Oyvind Ryeng
11-11-2017, 01:56 PM
The steel you are using is prone to galled or torn threads when cut at low surface speed. It may not be feasible to run fast enough to get a decent finish. In the shop where my son worked the shop foreman ordered the cheapest steel he could get to make some short shafts. In order to get sufficient speed to cut smoothly the RPM was so high the Z axis servo couldn't keep up, resulting in drunken threads. Try to get a steel better suited for machining. Others have posted their preferences. All are better suited for threading than what you use. Hot rolled and 0.2% carbon are a lousy combination.

Take a tip from pipe fitters. They die cut threads in really gummy steel all the time. They always use dark cutting oil that contains lots of sulfur. They seem to get decent threads at low speeds most of the time. Try the dark oil.

One of my favorite materials to machine is cold finished 1144 (Stressproof). Because of its sulfur content it is not recommended for welding.
Thanks for the tips. That's an interesting story regarding the drunken threads and servos that can't keep up. I've heard of Stressproof steel, but never seen it. At any rate, many of the things I make are welded after machining, and as such, general purpose mild steel is what I often use. I'd love to have some heat-treated 4140 or equivalent to experiment on. I do have some "hard" mystery steel that my Sandvik file will barely cut, but I've been too cheap to use it, and it's also mixed in with the rest of the mystery steel drops in cardboard boxes scattered along the floor.


I did some test runs on crappiest S355 cold drawn stock they sell around here.
HSS tool with couple of passes with 0.2mm plunging straight in:



Nasty nasty... decrease the cutting depth to 0.04mm per rev and 0.02mm for last 5 passes:



The one on the left is turned with HSS tool and the one on the right is turned with ER16 VP15TF carbide insert.
Took probably 3 times longer with the pretty sharp sharp HSS tooling because it was tearing a lot more compared to insert. Insert tool did tear some but it was nowhere near as bad.
On some parts of the thread the finish looks great on the piece turned with HSS tool but there is still tearing marks visible. .The one turned with insert has more constant finish from thread to thread but doesn't look as nice as the piece turned with HSS in the best parts.

Both run @100rpm and last few finishing passes @ 40rpm.
Very nice results, very nice. I especially liked the first image which looks like a mirror copy of my results. What diameter and pitch were you threading?


It sure looks like a case of bad material, since the SS turned out so nicely. Have you tried turning or facing the same material? If you have problems with that, it would definitely point to a material problem.

[...]

Here is my first attempt ever at threading, 3/8"-16, in a piece of steel (probably 1018):



This was done on my Harbor Freight 9x20 lathe using a hand-sharpened HSS tool bit. You can see that I may not have had the compound set quite right, so there are ridges for each pass. I think this is the threading tool I used:

Come on now, how can free material be bad? Things that are free are not given away because they cause more problems than they solve. Right? Nice results on your threading job!


Right below your cutting edge, looks like no clearance..
I mean the side toward the chuck.
Side rake on top of tool should be ok, just makes it harder to check with the guage while grinding.
I measured the clearance below the "primary" cutting edge by eye, and I got 5-6 degrees. That seems low to me, and I might have to try clamping a piece of steel on my bench grinder tool rest to cut more on the bottom of the tool for the next time.


I share the questions with regard to the very edge area where the honing is done. That must still have some clearance rake.

Also, the side is nice, but the top of the tool is not very good-looking. Maybe the edge is not as sharp as it could be as to the top. And also maybe the cut material is not getting away cleanly, and may be getting re-welded onto the part. It does not look like classic re-welding, but ......



But his back-side edge is obtuse angle, not a cutting angle. So making it try to cut is maybe not so good.

Also, something looks wrong with the pictures. The material that is smeared, looks like it is "smeared forward" with the rotation, and not "smeared back" in the direction the tool should have pushed it against rotation. Otherwise looks a bit like the way a built-up edge tears away.

And again, is the threading tool ground with slight angle to account for the thread helix? It does not always seem as if that would be so important, but.....
The honing on the top of my tool is not perfect, or even great, but I use a similar method on other HSS tools for general turning and they usually cut well. I might have too little clearance in the front (left side) of the cutting tool, I'll look into that.


This what I'm seeing as well, not sure if this is an artifact of the photo or not but this could be responsible for the torn effect left by the tool bit, especially in soft gummy steel. I have found that when cutting these types of steels that just the slightest variation of the cutting edge geometry can make a surprisingly huge difference in finish quality.

I see that the facing cut on the end of the work piece has a much more satisfactory finish. What can you do to the thread cutting tool bit to achieve similar geometry/results?

The facing cut was made by a Mitsubishi CNGG 120408 MJ VP15TF at a relatively slow surface speed and a "normal" feed. That's an interesting observation regarding small changes having a large impact. I guess one does not have a lot to lose by experimenting, maybe except in the area of hard drugs.


Take a piece of bar stock, put it in the chuck.
Now using your threading tool cut a wide chamfer with the tool.
Tell us what happens... if it can do that nicely it won't cut good threads....
Sorry, I forgot to try that today while I was out in the shop and running the lathe.


Just remember that you need to account for the helix angle. Some of the coarsest standard threads like 1/4-20 UNC have almost 4 degrees helix angle. If you grind the relief angle to 7 degrees you have effectively only 3 degrees relief angle left on the leading edge.
Good point, I'll have to look into this.



I had some free shop time today after I finished modifying a small Oilite (?) bushing for one of my customers International Harvester tractor transmission. I ground a new 60-degree included angle threading tool with the same 9-degree offset, but instead of giving it a side rake I instead ground in a back rake of about 10-12 degrees. The result was a somewhat improved finish, still threading at 125 RPM and feeding in @ 29.5 degrees between 0.20 - 0.02 mm. My photography got worse, however; I used my Samsung Galaxy S5 mobile phone instead of my DSLR. It actually has more megapixels, but megapixels aren't everything.

EDIT:
I only took one finish pass, the pass beforehand was probably fed in 0.05 - 0.06 mm. Do ye reckon' taking several finishing passes might have led to a better result?

http://oyvindryeng.net/img_host/threading/16.jpg

http://oyvindryeng.net/img_host/threading/17.jpg

EDIT2: Video filmed on my GoPro Hero 4, "narrow" angle of view. Random background music in the shop was supplied by Pantera for the occation. Note: the video is still uploading and will be ready about one hour from now on:

Direct link:
https://youtu.be/yZSJQYP0ddI

Embedded (maybe):

https://youtu.be/yZSJQYP0ddI

More embedding tries:


<iframe width="560" height="315" src="https://www.youtube.com/embed/yZSJQYP0ddI" frameborder="0" gesture="media" allowfullscreen></iframe>

MattiJ
11-11-2017, 02:47 PM
You definetely need more finishing passes. I did more than ten! 5 passes with 0.04mm DOC and five more passes at 0.02mm doc. Before that it looked just like yours.
And about M20 and 2,5mm pitch or something like that.

Oyvind Ryeng
11-11-2017, 03:27 PM
Very well, I'll make an effort to try that. Thanks for the clarification.

J Tiers
11-11-2017, 03:57 PM
Be careful with back rake, as that is what changes the effective cutting geometry, and thus the actual angle of thread that you cut.

Any time the top of the tool is not perfectly radial to the work, you will have a change of geometry vs what is ground into the tool. The more off of radial, the larger that effect is.

754
11-11-2017, 04:07 PM
If the material is tearing, allow .15mm for 3 or 4 finishing passes, it can clean up a lot of bad looks.
I never measure the angles of the side of my handground tool just the 60 degree part. Hold it to the work or another thread to see if it needs more clearance ..then when you hone you do a thin edge, NOT the WHOLE side.
Then when you touch up the tool later it's quicker.
I love threading I finally bought insert tooling for OD threadin
My lathe Had a very nice gearbox, easyvto use. I can remember setting up to thread say 3/8 or 1/2 inch, a short thread.. 8 minutes start to finish, for 1st thread.

Oyvind Ryeng
11-13-2017, 04:10 AM
Be careful with back rake, as that is what changes the effective cutting geometry, and thus the actual angle of thread that you cut.

Any time the top of the tool is not perfectly radial to the work, you will have a change of geometry vs what is ground into the tool. The more off of radial, the larger that effect is.
I realize this, and have already tested the geometry against a known good bolt, and the flank angles of the thread are by eye pretty close.



If the material is tearing, allow .15mm for 3 or 4 finishing passes, it can clean up a lot of bad looks.
I never measure the angles of the side of my handground tool just the 60 degree part. Hold it to the work or another thread to see if it needs more clearance ..then when you hone you do a thin edge, NOT the WHOLE side.
Then when you touch up the tool later it's quicker.
I love threading I finally bought insert tooling for OD threadin
My lathe Had a very nice gearbox, easyvto use. I can remember setting up to thread say 3/8 or 1/2 inch, a short thread.. 8 minutes start to finish, for 1st thread.
0.15 mm. sounds to me like a lot for a finishing pass. That's more like what I use for roughing. I guess you ment 0.015 mm?



At any rate, the problem is now mostly solved. I threaded a piece of mystery mild steel near 48 mm. OD @ 180 RPM with a 2.0 mm. pitch and had success. I also found me a ~60 mm. piece of some kind of harder mystery steel, perhaps chromium-molybdenum-alloy and also had success, AFTER losing the cutting edge once due to too high surface speed. I ended up at 90 RPM at this diameter and kept the edge throughout. I did not nearly get a mirror finish, but highly serviceable. Thank you all for your suggestions throughout this tough, trying time. I took ~20 minutes worth of uncommented video with my GoPro, let me know if you want to see this.

http://oyvindryeng.net/img_host/threading/18.jpg

754
11-13-2017, 05:29 AM
What I mean was 3 or 4 passes to do the last 6 thou,,or .15mm.
The blue chips in your last pic, were those from threading, if so, too fast.

Oyvind Ryeng
11-13-2017, 08:06 AM
What I mean was 3 or 4 passes to do the last 6 thou,,or .15mm.
The blue chips in your last pic, were those from threading, if so, too fast.
Oh, now I get it.

Those blue chips came from carbide tooling doing the undercut and turning and facing. When first threading this harder steel i got some dark gold / light brown chips and lost the cutting edge right after. Too fast, no doubt.

JoeLee
11-13-2017, 08:53 AM
Looks typical of HR or material with poor machining characteristics or too much give in the tool / holder etc.
Try cutting them on a piece of brass or alum and see what you get. Process of elimination.

JL................